Wind tunnel Boundary Conditions in Fluent
 

Hi friends
I've performed several tests in the open circuit suction wind tunnel (Fan at down stream) and now I want to simulate it by Fluent. A schematic of wind tunnel is like figure below:
http://ss1.spletnik.si/4_4/000/000/3...6_189_1701.jpg
(Figure is found on google.com)
As you now both sides of wind tunnel have atmospheric pressure, in simulation I have created the domain and model same as what I had in test section. for Boundary conditions, I selected Velocity inlet and pressure outlet which has 0 value for gauge pressure. But the solution is not correct. in my model the flow goes up because of suction inside the test section. (fan sucks air and increase the velocity) but simulation shows there is pressure rather than suction.
in other case I used pressure inlet and pressure outlet with 0 value for gauge pressure but in this case also the solution is not correct!
Mass flow inlet and pressure outlet also same as first case gives pressure rather than suction!
I have measured the velocity of air inside the test section by using pitot-static tube. Also static pressure inside the model were measured by pressure taps.
(a cube space house with windows on opposite walls with a chimney which only chimney was located inside the test section and other parts were located at outside of test section). for this model windows are pressure inlet with 0 value for gauge pressure.
I'm very confused how come I can manage my Boundary conditions to validate my results.
I would be appreciated if you share your useful experiences with me.
I have run the tests under different AOAs and velocities from 5 to 25 m/s.

pressure boundary conditions, wind tunnel, gauge pressure, pressure inlet
 

Hi !

I realise your post is almost a year old now, but your problem is very similar to mine; so rather than start a new thread, I will try to post my experience here, and hopefully also get some feedback.

I have a tunnel very similar to the one you picture, except that the intake duct is rather more crude, and for me - that is where the problem is. Choosing the right BC's for this geometry turned out to be less straight forward that I had assumed.

Attachment 41656

Without thinking twice about it, I also started with vel-inlet and pres-outlet conditions. I knew what bulk velocity I wanted at the test section so I obtained what inlet velocity I required at the inlet from continuity (subsonic flow). So I assigned inlet condition as an axial velocity component. This gave me the following velocity profiles (taken from the inlet at different stations, finishing at mid-test section).

Attachment 41653

You can see the profiles are totally unrealistic with that strange accelerating flow between the centreline and the walls. And the problem is I believe with the velocity inlet condition - it is incorrect I believe to force the inflow as an axial velocity because of the surface curvature. As you pointed out, the fan at the rear creates a low pressure and sucks air through the duct - which implies that a solution using only pressure BC's would be more realistic.

After a few attempts with combinations of fan/exhaust/press BCs, I have settled with pres-inlet and pres-outlet BCs. I left the gauge pressure for both surfaces at default 0 and only assigned a target mass-flow rate. It turns out that this seems to work. Or at least, I am getting much more realistic velocity profiles now:

Attachment 41658

without the weird near wall acceleration. After reading your post, I also looked at the static pressure, and it seems to be generating an under-pressure:

Attachment 41659

From what I recall from CFD programming though, for this flow regime, the pressure level is arbitrary as it is the pressure gradient that we solve for. In other words, the pressure level for this type of flow is non-unique, which is I think where the operating pressure setting comes in (default 1atm=101325Pa in Fluent, to establish the pressure level); the important quantity for the flow solution though being the pressure gradient.

Lastly, I'd like to report that with this implementation of pressure inlet and outlet, the solution oscillates wildly. It does appear to be converging (still has a few more iterations to go, but almost there), but does so with large overshoots:

Attachment 41660

I am not completely aware of how the pressure boundaries constrain the problem but it appears to be less stable. The fact the pressure adapts to the assigned target mass flow rate (despite zero gauge pressure at each end), is also a bit confusing and begs the question of the impact of the gauge pressure setting, since it seems to adapt anyway to the target mass flowrate. Any feedback about implementation of BCs and interpretation of the gauge pressure and results shown would be welcome!

Cheers!

P.S. An alternative approach to obtain a more realistic inflow profile was to patch a potential flow solution (inviscid calculation in fluent) for an arbitrary domain outside of the tunnel, but didn't get anywhere with that - plus it is not as robust as you'd have to adjust the solution every time.

Some general thoughts, not particular to anyone's problem.

Of course the best type of boundary conditions are conditions where you specify everything. But from a modelling standpoint, the pressure inlet & outlet boundary condition are the most physically accurate conditions for this type of problem. Actually a better inlet condition is to specify the inlet stagnation pressure to atmospheric and use a pressure outlet with targeted massflow rate if you know flowrate. The inlet stagnation pressure is atmospheric because flow is being induced from atmospheric pressure (hence the pressure at the inlet of the wind tunnel is sub-atmospheric and you can measure and verify this fact). It's also better to use the pressure profile option that allows the static pressure to vary over the plane.

The operating pressure is there to help reduce truncation error in the solver (since only the pressure gradient matter in the flow solution, for incompressible or compressible flow). The operating pressure should be near the mean pressure so that these pressure gradients can be computed with highest numerical accuracy (least truncation error). For high Mach number flows, pressure gradients are large and on the order of the operating pressure, so truncation error is not an issue but for low Mach number problems where the pressure gradients are small (the operating pressure can affect the quality of the computed result). Hence I would say the opposite and say that the operating pressure is most important for low Mach number simulations and less important for high Mach number. The operating pressure does not play a role if you use a constant density or temperature dependent density for your equation of state. If you use other equations of state however, then operating pressure is important for determining the changes in properties throughout your domain.

If you use a targeted mass flow rate, the gauge pressure is just an initial guess for the gauge pressure. If you have a good initial guess, you usually get faster solutions, otherwise the gauge pressure input is arbitrary since it is updated each iteration.

One issue with the targeted mass flow rate option is that the pressure is adjusted using a Bernoulli type approach. It also has a urf of 0.05. You can only change this urf through TUI and not the GUI. You can adjust the urf to improve the oscillations. The Bernoulli approach to adjust the massflow rate option can sometimes be opposite what you need. The Bernoulli approach is, if the calculated mass flow rate is less than the desired target, the outlet pressure is reduced (to increase the delta P between inlet and outlet). If the calculated massflow rate is too high, then the pressure is increased. If you have pressure dependent properties at this can cause you to converge to the wrong mass flow rate (since density increases with pressure, massflow tends to increase with pressure) and the solution tends to diverge. Then you have to change the urf to negative value (-0.05) to get it to work properly.

Hi guys,

I think this thread is tackling a similar issue to my simulation, although it's Star CCM+ rather than fluent.

I'm trying to replicate the buoyancy effects of the DeHaviland wind tunnel, from experimental data I'm expecting to see a drop in static pressure through the test section from -10Pa to -25Pa. However my simulation is dropping from 50 to 40Pa (guage). Can't seem to replicate the lower than atmospheric pressure values, regardless of mesh, anyone got any ideas on this?

Andrew

hi guys
thanks for the explanation
I have a question following this problem
What should I put for turbulent intensity and length scale for inlet and outlet of the wind tunnel
I am simulating Vertical Axis wind turbine

Hello Guys
Is the boundary conditions for inlet and outlet of the wind tunnel suppose to be equals?
I mean turbulent intensity and length scale.

In case someone is still looking for some pointers for this problem, consider the following:


Inlet BC: Mass-flow inlet works very well for this problem and is physically more valid since the job of the fan is to achieve a mass flow beyond taking care of losses.


Outlet BC: Pressure outlet works, especially with reduced gauge pressure by a value of the dynamic pressure across the fan. Can be calculated by taking area of fan section into account and applying AV = constant.


If you have a diffuser with some reasonable length and angle, a trick to get decent convergence is to initialize the domain with a velocity higher than the velocity at the exit of the diffuser (or the fan section). Initializing with contraction entry velocities may cause separation and reverse flow issues. This strategy has been tried in Fluent for a low speed case and works well.


All the best.